A Short SPICE Tutorial

Size: px
Start display at page:

Download "A Short SPICE Tutorial"

Transcription

1 A Short SPICE Tutorial Kenneth H. Carpenter Department of Electrical and Computer Engineering Kanas State University September 15, November 10, Introduction SPICE is an acronym for Simulation Program with Integrated Circuit Emphasis. There are many versions of this program, but all are based on the work done at the University of California at Berkeley[1], which resulted in two major, final versions: SPICE2G6 and SPICE3F4. Others have enhanced and extended (and fixed bugs) in these to produce new versions. Some of these are commercial; some are free software. In the following tutorial, the lowest common denominator of all the SPICE versions is described. That is, the SPICE input files will work with all the versions (known to the author). (Comments on how to extend the input files to take advantage of special features of special versions will be given in a few places.) SPICE uses a modified nodal analysis method[2] to solve electrical circuits. To communicate the topology of the circuit and the circuit values to SPICE one requires an input file containing a netlist. To communicate the analyses one requires from the program one places control lines in the input file. To obtain output from the analyses one places output control lines in the input file. The details of constructing this input file follow. 2 SPICE input file syntax All SPICE circuit simulators require an input file. This input file is an ASCII text file. The input file is line oriented. 1

2 2.1 Lines in a SPICE input file The first line of the file is a title to be placed on the output. It can contain any text. DO NOT FORGET that the first line in the file will be taken as the title and will not be used by SPICE in any other way, even if it is otherwise a valid control or netlist line. Any line that has an asterisk (*) in the first column is a comment. The entire line is ignored by SPICE (except for sometimes printing it in an output listing). Lines that are part of the netlist begin with an alphabetic character; the remainder of the line depends on the circuit element represented. Lines that control the SPICE program have a period (.) in the first column. Lines that have a plus sign (+) in the first column continue the previous line. That is, the SPICE program combines the characters in the line beginning with the plus sign with the previous line by discarding both the plus sign and the new line character(s) of the previous line. (It is wise to make continuation lines start where there is a natural break in the text.) Table 1 gives the SPICE input file for simulation of the circuit in Fig. 1. Table 1 illustrates the syntax described here. Fig. 1: Circuit schematic diagram for simulation of Table 1. 2

3 SPICE sample circuit - diode clamp *comment lines begin with asterisks *independent voltage source with DC value, AC value, and *transient square wave value: V AC 1 pulse e-8 1.e-8 1e-3 2e-3 *the square wave defined above has -10V to +20V extent, with *a period of 2 milliseconds *capacitor for clamping C e-6 *diode for clamp - model name is dclamp D1 2 0 dclamp *load resistor - large enought that RC >> 2 ms R e5 *model for diode.model dclamp D(IS=1e-14) *DC transfer function generated for this circuit.dc V *AC frequency sweep - assumes circuit is biased with V1 = 1V.AC OCT e2 1e4 *frequency is swept logarithmically from 100Hz to 10000Hz *transient analysis will show clamping.tran 1e-4 8e-3 0 1e-5 *start at time zero, go for 8 ms, make internal steps 10 microsec *save print data at.1 ms intervals *that s all folks.end Table 1: SPICE input file for sample simulation. 3

4 2.2 Divisions of a line in the SPICE input file The parser separates the characters on the input line into tokens. Tokens may be separated by blanks (space characters) an equals sign (=) (but only use these when you are giving a value to a parameter) a left or right parenthesis (but only use these when you are grouping following tokens) extra spaces are ignored Tokens can be either strings sequences of non-separator characters or numbers floating or fixed point decimal values as in c or FORTRAN e.g., 1.23e-5 or (Powers of ten can be indicated by adding one or more letters to the end of the number, without any intervening spaces, but don t do this as a beginner! See the SPICE User s Manual[3] for details.) 3 The SPICE netlist The part of the SPICE input file called the netlist describes the circuit to spice. In order to write a netlist one must have a circuit schematic with all nodes labeled. All nodes must have labels even nodes that connect only two circuit elements. There must be a ground node, and it must be labeled zero. For compatibility with all versions of SPICE, the node labels must be positive integers (except for ground which is node 0). 4

5 See Fig. 1 for an example of placing node labels on a schematic. Each circuit element must have a text label. The first letter of the label must be in the first column of the line for the circuit element in the netlist. The first letter specifies the type of circuit element it is. The rest of the letters and/or numbers of the label distinguish the different circuit elements of the same kind. Always use at least two characters for a circuit element label. These labels should be placed on the circuit schematic as in Fig. 1. The types of circuit elements and the first letters of their labels are as follows: V independent voltage source I independent current source R resistor C capacitor L inductor D diode Q bipolar junction transistor J JFET M MOSFET T lossless transmission line There are also letters to designate subcircuits, dependent sources, transmission lines, etc. See the SPICE User s Manual[3] or the on-line help files of the various SPICE versions for details of these other elements. A line in a SPICE input file representing a circuit element in the netlist has the following parts: The element label is the string identifying the element. It must begin with the letter identifying the element type in colunm one. After the circuit element label comes one or more spaces, then the label of the first node connected to the circuit element. 5

6 Then comes one or more spaces, then the label of the second node connected to the circuit element. If the circuit element connects to more than two nodes, then there are space separated node labels for all the nodes. After the node labels comes one or more spaces followed by the circuit element s value. Just how this value is expressed depends on the particular element. See below, or the SPICE User s Manual[3] or the on-line help files of the various SPICE versions for details of the values. 3.1 Value fields for circuit element lines R, L, and C lines These devices have as the first token the value field the number of their value. (in SI units - Ohms, Henries, or Farads). L and C elements may also have their initial conditions specified for transient analysis by a parameter token, IC, followed by a number token giving the initial value T lines A lossless transmission line requires specification of four nodes: two at the beginning of the line and two at the end. It also requires specification of the characteristic impedance and time delay of the line by giving them as parameters in the value field. A typical line in the netlist would be T Z0=50 TD=1E-6 This line has nodes 1 and 0 at the beginning and 2 and 0 at the end. The characteristic impedance is 50Ω and the time delay is 1µs. 3.2 V and I lines Independent sources can have a complicated set of value parameters given. The DC value of a source is either the first number after the last node label on the line, or it is the number following the token DC. The peak magnitude of the AC value of a source is the number following the token AC. (If the next token after AC is not a number then the 6

7 magnitude is taken as 1 and the phase as 0.) If the next token after the magnitude number is a number, it is the phase of the phasor. If the next token is not a number, the phase is zero. If a source is to be present in a circuit but have an AC value of zero, then the AC token must not appear on the line. A source to be used in a transient analysis has a function of time specified as the last set of tokens on the line. This function of time has several possible forms. See the SPICE User s Manual[3] for details. A single source can have any or all of the DC, AC, and function of time values. 3.3 D, Q, J and M lines These semiconductor devices must have models. The first token after the last node label must be a string which identifies the model. Following this token there can be other strings and numbers which modify the parameters of the model and set initial conditions. See the SPICE User s Manual[3] for details. When a line for each circuit element in the schematic is present then the netlist is complete. The Table 1 for an example. 4 Control lines in the SPICE input file All other lines, besides comments, title, and netlist lines, in the SPICE input file are control lines. Control lines all have a period (.) in the first column. There are many different control lines. They can be grouped as follows:.end line must be the last line in the input file analysis lines specify what simulations are to be performed include lines used to nest input files (not needed in simple applications) option lines set parameters and conditions for simulations, models, etc. output lines determine how output from simulations is to be presented 7

8 .model lines define the strings used as model parameters for circuit elements in the netlist 4.1.end line Although some SPICE versions may work without it, most require that a line consisting of just.end be the last line in the input file. 4.2 analysis lines There are many possible types of analyses. See the SPICE User s Manual[3] for all of them and for details of the following ones..dc line this causes a sweep of one or more voltage source DC values to be performed and the corresponding node voltages and source currents to be calculated to yield DC transfer functions..dc V would cause the source labeled V1 to have its value swept from -5 volts to +12 volts in steps of.1 volt. The DC value on the V1 line of the netlist would be ignored..ac line this causes a frequency sweep of all the independent sources having an AC token..ac V1 LIN would cause phasor analysis of the circuit to be performed for frequencies from 30 to 130 Hertz. 5 frequencies would be used. They would be separated linearly, that is by equal increments. Values of node voltages and source currents will be saved as complex numbers..tran line this causes a transient analysis to be performed..tran would cause time to be varied from an initial value of 0.05 seconds in internal steps not to exceed seconds until the stop time of 0.01 seconds is reached. Printed output of node voltages and currents can be obtained in steps of seconds. If a token UIC is appended, then the initial conditions specified in the netlist will be used. Otherwise a DC analysis will be performed to obtain the initial conditions. 8

9 4.3.model lines When a model is specified on a netlist line, there must be a corresponding.model line in the input file to define that model. The tokens on that line are as follows: The first token on the line is.model The second token on the line is the same string as used in the circuit element line of the netlist to name the model. The third token on the line identifies what kind of a model it is. D for diode NPN for NPN BJT PNP for PNP BJT NMOS for n channel MOSFET and so on. The remaining tokens on the line give the model parameters values when other than the defaults are required. See the SPICE User s Manual[3] for the parameters that go with each model and for their default values. 4.4 output lines print To obtain printed sets of node voltages and currents from simulations one includes control cards beginning with.print. For example.print AC V(2) will cause a table of values to be placed in the SPICE output file having the frequencies used in the AC analysis in the first column and the complex values of the voltage at node 2 in the second column plot Lines beginning with.plot work like.print lines except that instead of a table of values a printer plot is placed in the output file. This method of obtaining plots of output values is obsolete. Today one will use a graphical post processing program to produce the plots. With 9

10 PSpice, one puts a control line with the single token.probe into the input file in order to generate the output needed by the post processor, which is called Probe. BUT A LINE.probe MAY NOT APPEAR in the input file for any other verions of SPICE. Other versions of SPICE automatically output a file for graphical post processing without a line in the input file. 4.5 option lines There are many options that may be given to SPICE. These are too numerous to mention in a beginning tutorial. Most simulations will not need any of them. See the SPICE User s Manual[3] for a list of them. 4.6 include lines These lines allow other files to be nested inside the SPICE input file. The syntax of these lines depends on the particular versio of SPICE and the operating system. They are not needed for simple simulations. 5 Sample problem The SPICE input file of Table 1, based on the circuit shown in Fig. 1, can be input to a version of SPICE and the simulations in the control lines carried out. When this is done using PSpice, the output file shown in Table 5 is obtained. If a.probe line had been included in the input file, then the graphical data saved for the DC transfer function anaylsis could be plotted with Probe to obtain the plot in Fig. 2. **** 09/15/03 10:01:23 *********** Evaluation PSpice (Nov 1999) ************** SPICE sample circuit - diode clamp **** CIRCUIT DESCRIPTION ****************************************************************************** *comment lines begin with asterisks 10

11 *independent voltage source with DC value, AC value, and *transient square wave value: V AC 1 pulse e-8 1.e-8 1e-3 2e-3 *the square wave defined above has -10V to +20V extent, with *a period of 2 milliseconds *capacitor for clamping C e-6 *diode for clamp - model name is dclamp D1 2 0 dclamp *load resistor - large enought that RC >> 2 ms R e5 *model for diode.model dclamp D(IS=1e-14) *DC transfer function generated for this circuit.dc V *AC frequency sweep - assumes circuit is biased with V1 = 1V.AC OCT e2 *frequency is swept logarithmically from 100Hz to 10000Hz *transient analysis will show clamping.tran 1e-4 8e-3 0 1e-5 *start at time zero, go for 8 ms, make internal steps 10 microsec *save print data at.1 ms intervals.probe *that s all folks.end **** 09/15/03 10:01:23 *********** Evaluation PSpice (Nov 1999) ************** SPICE sample circuit - diode clamp **** Diode MODEL PARAMETERS ****************************************************************************** IS dclamp E-15 **** 09/15/03 10:01:23 *********** Evaluation PSpice (Nov 1999) ************** SPICE sample circuit - diode clamp 11

12 **** SMALL SIGNAL BIAS SOLUTION TEMPERATURE = DEG C ****************************************************************************** NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE ( 1) ( 2)-90.12E-27 VOLTAGE SOURCE CURRENTS NAME CURRENT V E+00 TOTAL POWER DISSIPATION 0.00E+00 WATTS **** 09/15/03 10:01:23 *********** Evaluation PSpice (Nov 1999) ************** SPICE sample circuit - diode clamp **** INITIAL TRANSIENT SOLUTION TEMPERATURE = DEG C ****************************************************************************** NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE ( 1) ( 2)-90.12E-27 VOLTAGE SOURCE CURRENTS NAME CURRENT V E+00 TOTAL POWER DISSIPATION 0.00E+00 WATTS JOB CONCLUDED TOTAL JOB TIME.75 12

13 Table 2. PSpice output file when file of Table 1 (with a.probe line added) is the input file. If the SPICE input file of Table 1 is run with WinSpice or Spice3 then there is no text output file generated. Instead to see the printed values obtained with PSpice by the.print statement, one gives the print command interactively. To see the plot like that from probe, one gives the plot command interactively. Table 3 contains the terminal session from using spice3f5 under Linux. It shows how the printed values may be observed and how plots are called. The plot of v(2) vs v(1) for the transient analysis is shown in Fig. 3. The student should try the input file of Table 1 in all three versions of SPICE to compare them. Then read further in the SPICE User s Manual and consult the web pages linked to the class web page for more information. 13

14 Fig. 2: Probe screen showing transient simulation from PSpice when input file is that given in Table 1 (with a.probe line added). 14

15 Script started on Mon Sep 15 11:12: elmo{khc}~/classes/525/spicetut:1> spice3 sample.cir Program: Spice, version: 3f5 Date built: Wed Aug 25 16:14:15 CDT 1999 Type "help" for more information, "quit" to leave. Circuit: SPICE sample circuit - diode clamp Spice 1 -> run Spice 2 -> setplot Type the name of the desired plot: new Current tran1 dc1 ac1 const? ac1 Spice 3 -> print v(2) New plot SPICE sample circuit - diode clamp (Transient Analysis) SPICE sample circuit - diode clamp (DC transfer characteristic) SPICE sample circuit - diode clamp (AC Analysis) Constant values (constants) SPICE sample circuit - diode clamp AC Analysis Mon Sep 15 11:12: Index frequency v(2) e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e e+01, e e-01, e hit return for more,? for help -- q Spice 4 -> setplot tran1 Spice 5 -> plot v(2) v(1) Spice 6 -> quit Table 3: Interactive session for spice3 simulation of input file in Table 1. 15

16 Fig. 3: Interactive plot from spice3 for transient simulation of input file in Table 1. 16

17 6 Transmission line sample problem SPICE provides a convenient way to visualize transients on transmission lines. Suppose one wishes to examine voltage and currents as a function of time at the ends and midpoint of a line. Then the schematic of Fig. 4 may be used. In Fig. 4 the transmission line is simulated as two transmission Fig. 4: Schematic for transmission line simulation using SPICE. lines in series, each with half the length of the total line. The voltage source between the lines will act as an ammeter to show current halfway along the line. A netlist using this schematic with a 5 volt step function input for VG is given in Table 4. Running the input file in Table 4 with Spice3 Sample transmission line simulation with unit step input VG 1 0 pwl 0 0 1e-10 5 RG T z0=50 td=5e-9 VI T z0=50 td=5e-9 VI RL tran 1e-10 1e-7 0 1e-10.end Table 4: SPICE netlist for transmission line example, based on schematic of Fig. 4. and plotting the current and voltage at the center of the line (by command plot v(3) 100*i(vi1)) yields the curves in Fig

18 Fig. 5: Plot of voltage and current at midpoint of transmission line shown in Fig. 4 using Spice3 with the input file shown in Table 4. 18

19 References [1] T. Perry, Donald O. Pederson [electronic engineering biography], IEEE Spectrum, Vol. 35, No. 6, pp , June [2] Laurence W. Nagel, SPICE2: A Computer Program to Simulate Semiconductor Circuits, Memorandum No. ERL-M520, Electronics Research Laboratory, College of Engineering, University of California, Berkeley, May 9, [3] T. Quarles, A. R. Newton, D.O.Pederson, A.Sangiovanni-Vincentelli, SPICE3 Version 3f3 User s Manual, Department of Electrical Engineering and Computer Sciences, University of California, Berkeley, Ca.. May

Introduction to PSpice

Introduction to PSpice Electric Circuit I Lab Manual 4 Session # 5 Introduction to PSpice 1 PART A INTRODUCTION TO PSPICE Objective: The objective of this experiment is to be familiar with Pspice (learn how to connect circuits,

More information

HSPICE (from Avant!) offers a more robust, commercial version of SPICE. PSPICE is a popular version of SPICE, available from Orcad (now Cadence).

HSPICE (from Avant!) offers a more robust, commercial version of SPICE. PSPICE is a popular version of SPICE, available from Orcad (now Cadence). Electronics II: SPICE Lab ECE 09.403/503 Team Size: 2-3 Electronics II Lab Date: 3/9/2017 Lab Created by: Chris Frederickson, Adam Fifth, and Russell Trafford Introduction SPICE (Simulation Program for

More information

The default account setup for the class should allow you to run HSPICE without any further configuration. To verify this, type:

The default account setup for the class should allow you to run HSPICE without any further configuration. To verify this, type: UNIVERSITY OF CALIFORNIA College of Engineering Department of Electrical Engineering and Computer Sciences HW #1: Circuit Simulation NTU IC541CA (Spring 2004) 1 Objective The objective of this homework

More information

WinSpice. The steps to performing a circuit simulation with WinSpice are:

WinSpice. The steps to performing a circuit simulation with WinSpice are: WinSpice Tutorial 1 A. Introduction WinSpice SPICE is short for Simulation Program with Integrated Circuit Emphasis. SPICE is a general-purpose circuit simulation program for nonlinear dc, nonlinear transient,

More information

Circuit Simulation with SPICE OPUS

Circuit Simulation with SPICE OPUS Circuit Simulation with SPICE OPUS Theory and Practice Tadej Tuma Arpäd Bürmen Birkhäuser Boston Basel Berlin Contents Abbreviations About SPICE OPUS and This Book xiii xv 1 Introduction to Circuit Simulation

More information

Introduction to SwitcherCAD

Introduction to SwitcherCAD Introduction to SwitcherCAD 1 PREFACE 1.1 What is SwitcherCAD? SwitcherCAD III is a new Spice based program that was developed for modelling board level switching regulator systems. The program consists

More information

Engineering 3821 Fall Pspice TUTORIAL 1. Prepared by: J. Tobin (Class of 2005) B. Jeyasurya E. Gill

Engineering 3821 Fall Pspice TUTORIAL 1. Prepared by: J. Tobin (Class of 2005) B. Jeyasurya E. Gill Engineering 3821 Fall 2003 Pspice TUTORIAL 1 Prepared by: J. Tobin (Class of 2005) B. Jeyasurya E. Gill 2 INTRODUCTION The PSpice program is a member of the SPICE (Simulation Program with Integrated Circuit

More information

ECE 201 LAB 6 INTRODUCTION TO SPICE/PSPICE

ECE 201 LAB 6 INTRODUCTION TO SPICE/PSPICE Version 1.1 1 of 33 BEFORE YOU BEGIN PREREQUISITE LABS Resistive Circuits EXPECTED KNOWLEDGE ECE 201 LAB 6 INTRODUCTION TO SPICE/PSPICE Ohm's Law: v = ir Node Voltage and Mesh Current Methods of Circuit

More information

Lab 3: Circuit Simulation with PSPICE

Lab 3: Circuit Simulation with PSPICE Page 1 of 11 Laboratory Goals Introduce text-based PSPICE as a design tool Create transistor circuits using PSPICE Simulate output response for the designed circuits Introduce the Curve Tracer functionality.

More information

THE SPICE BOOK. Andrei Vladimirescu. John Wiley & Sons, Inc. New York Chichester Brisbane Toronto Singapore

THE SPICE BOOK. Andrei Vladimirescu. John Wiley & Sons, Inc. New York Chichester Brisbane Toronto Singapore THE SPICE BOOK Andrei Vladimirescu John Wiley & Sons, Inc. New York Chichester Brisbane Toronto Singapore CONTENTS Introduction SPICE THE THIRD DECADE 1 1.1 THE EARLY DAYS OF SPICE 1 1.2 SPICE IN THE 1970s

More information

Laboratory Lecture 4

Laboratory Lecture 4 Gheorghe Asachi Technical University of Iasi Faculty of Electronics, Telecommunications and Information Technology Title of Discipline: Computer-Aided Analysis of Electronic Circuits Laboratory Lecture

More information

NGSPICE- Usage and Examples

NGSPICE- Usage and Examples NGSPICE- Usage and Examples Debapratim Ghosh deba21pratim@gmail.com Electronic Systems Group Department of Electrical Engineering Indian Institute of Technology Bombay February 2013 Debapratim Ghosh Dept.

More information

An Introductory Guide to Circuit Simulation using NI Multisim 12

An Introductory Guide to Circuit Simulation using NI Multisim 12 School of Engineering and Technology An Introductory Guide to Circuit Simulation using NI Multisim 12 This booklet belongs to: This document provides a brief overview and introductory tutorial for circuit

More information

Experiment 2 Introduction to PSpice

Experiment 2 Introduction to PSpice Experiment 2 Introduction to PSpice W.T. Yeung and R.T. Howe UC Berkeley EE 105 Fall 2004 1.0 Objective One of the CAD tools you will be using as a circuit designer is SPICE, a Berkeleydeveloped industry-standard

More information

PSpice Simulation. The target of computer-aided analysis is to determine the circuit currents and voltages everywhere in the circuit.

PSpice Simulation. The target of computer-aided analysis is to determine the circuit currents and voltages everywhere in the circuit. PSpice Simulation The target of computer-aided analysis is to determine the circuit currents and voltages everywhere in the circuit. For PSpice, the circuit is described by a text file called the netlist.

More information

SPICE FOR POWER ELECTRONICS AND ELECTRIC POWER

SPICE FOR POWER ELECTRONICS AND ELECTRIC POWER SPICE FOR POWER ELECTRONICS AND ELECTRIC POWER SECOND EDITION MUHAMMAD H. RASHID University of West Florida Pensacola, Florida, U.S.A. HASAN M. RASHID University of Florida Gainesville, Florida, U.S.A.

More information

5.25Chapter V Problem Set

5.25Chapter V Problem Set 5.25Chapter V Problem Set P5.1 Analyze the circuits in Fig. P5.1 and determine the base, collector, and emitter currents of the BJTs as well as the voltages at the base, collector, and emitter terminals.

More information

Experiment 6: Biasing Circuitry

Experiment 6: Biasing Circuitry 1 Objective UNIVERSITY OF CALIFORNIA AT BERKELEY College of Engineering Department of Electrical Engineering and Computer Sciences EE105 Lab Experiments Experiment 6: Biasing Circuitry Setting up a biasing

More information

Pulsed Power Engineering Circuit Simulation

Pulsed Power Engineering Circuit Simulation Pulsed Power Engineering Circuit Simulation January 12-16, 2009 Craig Burkhart, PhD Power Conversion Department SLAC National Accelerator Laboratory Circuit Simulation for Pulsed Power Applications Uses

More information

EE320L Electronics I. Laboratory. Laboratory Exercise #6. Current-Voltage Characteristics of Electronic Devices. Angsuman Roy

EE320L Electronics I. Laboratory. Laboratory Exercise #6. Current-Voltage Characteristics of Electronic Devices. Angsuman Roy EE320L Electronics I Laboratory Laboratory Exercise #6 Current-Voltage Characteristics of Electronic Devices By Angsuman Roy Department of Electrical and Computer Engineering University of Nevada, Las

More information

Group of Institutions

Group of Institutions Group of Institutions ELECTRICAL SIMULATION LABORATORY MANUAL (EEE-453) DEPARTMENT OF ELECTRICAL & ELECTRONICS ENGINEERING 27, Knowledge Park-III, Greater Noida, (U.P.) Phone : 0120-2323854-58 website

More information

EXPERIMENT 9 Problem Solving: First-order Transient Circuits

EXPERIMENT 9 Problem Solving: First-order Transient Circuits EXPERIMENT 9 Problem Solving: First-order Transient Circuits I. Introduction In transient analyses, we determine voltages and currents as functions of time. Typically, the time dependence is demonstrated

More information

Experiment 6: Biasing Circuitry

Experiment 6: Biasing Circuitry 1 Objective UNIVERSITY OF CALIFORNIA AT BERKELEY College of Engineering Department of Electrical Engineering and Computer Sciences EE105 Lab Experiments Experiment 6: Biasing Circuitry Setting up a biasing

More information

SPICE for Power Electronics and Electric Power

SPICE for Power Electronics and Electric Power SPICE for Power Electronics and Electric Power Third Edition Muhammad H. Rashid Life Fellow IEEE /^0\ \Cf*' CRC Press I Taylor & Francis eis Crou Group Boca Raton London New York CRC Press is an imprint

More information

PHYS 3152 Methods of Experimental Physics I E2. Diodes and Transistors 1

PHYS 3152 Methods of Experimental Physics I E2. Diodes and Transistors 1 Part I Diodes Purpose PHYS 3152 Methods of Experimental Physics I E2. In this experiment, you will investigate the current-voltage characteristic of a semiconductor diode and examine the applications of

More information

Lab #2 First Order RC Circuits Week of 27 January 2015

Lab #2 First Order RC Circuits Week of 27 January 2015 ECE214: Electrical Circuits Laboratory Lab #2 First Order RC Circuits Week of 27 January 2015 1 Introduction In this lab you will investigate the magnitude and phase shift that occurs in an RC circuit

More information

ET 304A Laboratory Tutorial-Circuitmaker For Transient and Frequency Analysis

ET 304A Laboratory Tutorial-Circuitmaker For Transient and Frequency Analysis ET 304A Laboratory Tutorial-Circuitmaker For Transient and Frequency Analysis All circuit simulation packages that use the Pspice engine allow users to do complex analysis that were once impossible to

More information

PSPICE T UTORIAL P ART I: INTRODUCTION AND DC ANALYSIS. for the Orcad PSpice Release 9.2 Lite Edition

PSPICE T UTORIAL P ART I: INTRODUCTION AND DC ANALYSIS. for the Orcad PSpice Release 9.2 Lite Edition PSPICE T UTORIAL P ART I: INTRODUCTION AND DC ANALYSIS for the Orcad PSpice Release 9.2 Lite Edition INTRODUCTION The Simulation Program with Integrated Circuit Emphasis (SPICE) circuit simulation tool

More information

A Brief Handout for Introduction to

A Brief Handout for Introduction to A Brief Handout for Introduction to Electric cal Engineering Course This handout is a compilation of PSPICE, A Brief Primer, Department of Electrical and Systems Engineering, University of Pennsylvania

More information

INTRODUCTION TO CIRCUIT SIMULATION USING SPICE

INTRODUCTION TO CIRCUIT SIMULATION USING SPICE LSI Circuits INTRODUCTION TO CIRCUIT SIMULATION USING SPICE Introduction: SPICE (Simulation Program with Integrated Circuit Emphasis) is a very powerful and probably the most widely used simulator for

More information

EXPERIMENT 5 CURRENT AND VOLTAGE CHARACTERISTICS OF BJT

EXPERIMENT 5 CURRENT AND VOLTAGE CHARACTERISTICS OF BJT EXPERIMENT 5 CURRENT AND VOLTAGE CHARACTERISTICS OF BJT 1. OBJECTIVES 1.1 To practice how to test NPN and PNP transistors using multimeter. 1.2 To demonstrate the relationship between collector current

More information

Using LTSPICE to Analyze Circuits

Using LTSPICE to Analyze Circuits Using LTSPICE to Analyze Circuits Overview: LTSPICE is circuit simulation software that automatically constructs circuit equations using circuit element models (built in or downloadable). In its modern

More information

UNIT 3: FIELD EFFECT TRANSISTORS

UNIT 3: FIELD EFFECT TRANSISTORS FIELD EFFECT TRANSISTOR: UNIT 3: FIELD EFFECT TRANSISTORS The field effect transistor is a semiconductor device, which depends for its operation on the control of current by an electric field. There are

More information

4 Transistors. 4.1 IV Relations

4 Transistors. 4.1 IV Relations 4 Transistors Due date: Sunday, September 19 (midnight) Reading (Bipolar transistors): HH sections 2.01-2.07, (pgs. 62 77) Reading (Field effect transistors) : HH sections 3.01-3.03, 3.11-3.12 (pgs. 113

More information

Electrical, Electronic and Communications Engineering Technology/Technician CIP Task Grid

Electrical, Electronic and Communications Engineering Technology/Technician CIP Task Grid Secondary Task List 100 SAFETY 101 Describe OSHA safety regulations. 102 Identify, select, and demonstrate proper hand tool use for electronics work. 103 Recognize the types and usages of fire extinguishers.

More information

Mentor Analog Simulators

Mentor Analog Simulators ENGR-434 Spice Netlist Syntax Details Introduction Rev 5/25/11 As you may know, circuit simulators come in several types. They can be broadly grouped into those that simulate a circuit in an analog way,

More information

Unit/Standard Number. LEA Task # Alignment

Unit/Standard Number. LEA Task # Alignment 1 Secondary Competency Task List 100 SAFETY 101 Demonstrate an understanding of State and School safety regulations. 102 Practice safety techniques for electronics work. 103 Demonstrate an understanding

More information

Department of Electrical & Computer Engineering Technology. EET 3086C Circuit Analysis Laboratory Experiments. Masood Ejaz

Department of Electrical & Computer Engineering Technology. EET 3086C Circuit Analysis Laboratory Experiments. Masood Ejaz Department of Electrical & Computer Engineering Technology EET 3086C Circuit Analysis Laboratory Experiments Masood Ejaz Experiment # 1 DC Measurements of a Resistive Circuit and Proof of Thevenin Theorem

More information

Using LTspice a Short Intro with Examples

Using LTspice a Short Intro with Examples Using LTspice a Short Intro with Examples LTspice, also called SwitcherCAD, is a powerful and easy to use schematic capture program and SPICE engine, which is a general-purpose circuit simulation program

More information

E B C. Two-Terminal Behavior (For testing only!) TO-92 Case Circuit Symbol

E B C. Two-Terminal Behavior (For testing only!) TO-92 Case Circuit Symbol Physics 310 Lab 5 Transistors Equipment: Little silver power-supply, little black multimeter, Decade Resistor Box, 1k,, 470, LED, 10k, pushbutton switch, 270, 2.7k, function generator, o scope, two 5.1k

More information

Laboratory #2 PSpice Analyses

Laboratory #2 PSpice Analyses Laboratory #2 PSpice Analyses I. Objectives 1. Know the development of SPICE. 2. Learn to install the PSpice software. 3. Learn to use the Capture CIS to draw circuit. 4. Learn to use the four analyses

More information

Introduction to OrCAD. Simulation Program With Integrated Circuits Emphasis.

Introduction to OrCAD. Simulation Program With Integrated Circuits Emphasis. Islamic University of Gaza Faculty of Engineering Electrical Engineering department Digital Electronics Lab (EELE 3121) Eng. Mohammed S. Jouda Eng. Amani S. abu reyala Experiment 1 Introduction to OrCAD

More information

ELEC 2210 EXPERIMENT 7 The Bipolar Junction Transistor (BJT)

ELEC 2210 EXPERIMENT 7 The Bipolar Junction Transistor (BJT) ELEC 2210 EXPERIMENT 7 The Bipolar Junction Transistor (BJT) Objectives: The experiments in this laboratory exercise will provide an introduction to the BJT. You will use the Bit Bucket breadboarding system

More information

Well we know that the battery Vcc must be 9V, so that is taken care of.

Well we know that the battery Vcc must be 9V, so that is taken care of. HW 4 For the following problems assume a 9Volt battery available. 1. (50 points, BJT CE design) a) Design a common emitter amplifier using a 2N3904 transistor for a voltage gain of Av=-10 with the collector

More information

EE320L Electronics I. Laboratory. Laboratory Exercise #2. Basic Op-Amp Circuits. Angsuman Roy. Department of Electrical and Computer Engineering

EE320L Electronics I. Laboratory. Laboratory Exercise #2. Basic Op-Amp Circuits. Angsuman Roy. Department of Electrical and Computer Engineering EE320L Electronics I Laboratory Laboratory Exercise #2 Basic Op-Amp Circuits By Angsuman Roy Department of Electrical and Computer Engineering University of Nevada, Las Vegas Objective: The purpose of

More information

Fig. 1-1 show the main window of Orcad Capture. Every project you work on will start from Orcad Capture. Fig. 1-1 Orcad Capture Main window.

Fig. 1-1 show the main window of Orcad Capture. Every project you work on will start from Orcad Capture. Fig. 1-1 Orcad Capture Main window. T. K. Ha PSpice Lecture #1 1 Objective: By the end of this lecture, it is hope that the students will have a rudimentary knowledge of using and running PSpice. The student will be able to draw and edit

More information

Tsung-Chu Huang. Department of Electronic Engineering National Changhua University of Education /10/4-5 TCH NCUE

Tsung-Chu Huang. Department of Electronic Engineering National Changhua University of Education /10/4-5 TCH NCUE Digital IC Design Tsung-Chu Huang Department of Electronic Engineering National Changhua University of Education Email: tch@cc.ncue.edu.tw 2004/10/4-5 Page 1 Circuit Simulation Tools 1. Switch Level: Verilog,

More information

MASSACHUSETTS INSTITUTE OF TECHNOLOGY Department of Electrical Engineering and Computer Science Microelectronic Devices and Circuits Fall 2009

MASSACHUSETTS INSTITUTE OF TECHNOLOGY Department of Electrical Engineering and Computer Science Microelectronic Devices and Circuits Fall 2009 1 MASSACHUSETTS INSTITUTE OF TECHNOLOGY Department of Electrical Engineering and Computer Science 6.012 Microelectronic Devices and Circuits Fall 2009 SPECIAL PROBLEM ON CIRCUIT DESIGN 12/1/09 edition

More information

Impedance of HART Transmitters Nesebar, Inc.

Impedance of HART Transmitters Nesebar, Inc. Impedance of HART Transmitters Nesebar, Inc. A 2Wire 420 ma Process Transmitter is essentially a current regulator. The compliance impedance of the regulator is often tens of megohms near DC but drops

More information

Curve Tracer Laboratory Assistant Using the Analog Discovery Module as A Curve Tracer

Curve Tracer Laboratory Assistant Using the Analog Discovery Module as A Curve Tracer Curve Tracer Laboratory Assistant Using the Analog Discovery Module as A Curve Tracer The objective of this lab is to become familiar with methods to measure the dc current-voltage (IV) behavior of diodes

More information

ES 330 Electronics II Homework # 1 (Fall 2016 SOLUTIONS)

ES 330 Electronics II Homework # 1 (Fall 2016 SOLUTIONS) SOLUTIONS ES 330 Electronics II Homework # 1 (Fall 2016 SOLUTIONS) Problem 1 (20 points) We know that a pn junction diode has an exponential I-V behavior when forward biased. The diode equation relating

More information

ES 330 Electronics II Homework # 2 (Fall 2016 Due Wednesday, September 7, 2016)

ES 330 Electronics II Homework # 2 (Fall 2016 Due Wednesday, September 7, 2016) Page1 Name ES 330 Electronics II Homework # 2 (Fall 2016 Due Wednesday, September 7, 2016) Problem 1 (15 points) You are given an NMOS amplifier with drain load resistor R D = 20 k. The DC voltage (V RD

More information

5 Introduction to SPICE

5 Introduction to SPICE 5 Introduction to SPICE This session demonstrates the operation and use of SPICE3F. The aspects introduced are the interactive shell, netlists, and basic simulations. 5.1 Equipment 1 SPICE Access to WinSPICE

More information

EXPERIMENT NUMBER 10 TRANSIENT ANALYSIS USING PSPICE

EXPERIMENT NUMBER 10 TRANSIENT ANALYSIS USING PSPICE EXPERIMENT NUMBER 10 TRANSIENT ANALYSIS USING PSPICE Objective: To learn to use a circuit simulator package for plotting the response of a circuit in the time domain. Preliminary: Revise laboratory 8 to

More information

JFET 101, a Tutorial Look at the Junction Field Effect Transistor 8May 2007, edit 2April2016, Wes Hayward, w7zoi

JFET 101, a Tutorial Look at the Junction Field Effect Transistor 8May 2007, edit 2April2016, Wes Hayward, w7zoi JFET 101, a Tutorial Look at the Junction Field Effect Transistor 8May 2007, edit 2April2016, Wes Hayward, w7zoi FETs are popular among experimenters, but they are not as universally understood as the

More information

Experiment 9 Bipolar Junction Transistor Characteristics

Experiment 9 Bipolar Junction Transistor Characteristics Experiment 9 Bipolar Junction Transistor Characteristics W.T. Yeung, W.Y. Leung, and R.T. Howe UC Berkeley EE 105 Fall 2005 1.0 Objective In this lab, you will determine the I C - V CE characteristics

More information

Lab 2: Discrete BJT Op-Amps (Part I)

Lab 2: Discrete BJT Op-Amps (Part I) Lab 2: Discrete BJT Op-Amps (Part I) This is a three-week laboratory. You are required to write only one lab report for all parts of this experiment. 1.0. INTRODUCTION In this lab, we will introduce and

More information

SAMPLE FINAL EXAMINATION FALL TERM

SAMPLE FINAL EXAMINATION FALL TERM ENGINEERING SCIENCES 154 ELECTRONIC DEVICES AND CIRCUITS SAMPLE FINAL EXAMINATION FALL TERM 2001-2002 NAME Some Possible Solutions a. Please answer all of the questions in the spaces provided. If you need

More information

A SPICE (PSPICE) Tutorial

A SPICE (PSPICE) Tutorial APPENDIX D A SPICE (PSPICE) Tutorial This is a brief summary of the SPICE, or its personal computer version PSPICE, electric circuit analysis program. SPICE is an acronym for simulation program with integrated-circuit

More information

RLC Frequency Response

RLC Frequency Response 1. Introduction RLC Frequency Response The student will analyze the frequency response of an RLC circuit excited by a sinusoid. Amplitude and phase shift of circuit components will be analyzed at different

More information

LABORATORY 7 v2 BOOST CONVERTER

LABORATORY 7 v2 BOOST CONVERTER University of California Berkeley Department of Electrical Engineering and Computer Sciences EECS 100, Professor Bernhard Boser LABORATORY 7 v2 BOOST CONVERTER In many situations circuits require a different

More information

Experiment #1 Introduction to SPICE

Experiment #1 Introduction to SPICE Jonathan Roderick Experiment #1 Introduction to SPICE Introduction: This experiment is designed to familiarize the student with SPICE. SPICE simulations will be needed for prelabs and projects contained

More information

Paper-1 (Circuit Analysis) UNIT-I

Paper-1 (Circuit Analysis) UNIT-I Paper-1 (Circuit Analysis) UNIT-I AC Fundamentals & Kirchhoff s Current and Voltage Laws 1. Explain how a sinusoidal signal can be generated and give the significance of each term in the equation? 2. Define

More information

Lab 3: BJT Digital Switch

Lab 3: BJT Digital Switch Lab 3: BJT Digital Switch Objectives The purpose of this lab is to acquaint you with the basic operation of bipolar junction transistor (BJT) and to demonstrate its functionality in digital switching circuits.

More information

Introduction to Pspice

Introduction to Pspice 1. Objectives Introduction to Pspice The learning objectives for this laboratory are to give the students a brief introduction to using Pspice as a tool to analyze circuits and also to demonstrate the

More information

ECEN 325 Lab 7: Characterization and DC Biasing of the BJT

ECEN 325 Lab 7: Characterization and DC Biasing of the BJT ECEN 325 Lab 7: Characterization and DC Biasing of the BJT 1 Objectives The purpose of this lab is to characterize NPN and PNP bipolar junction transistors (BJT), and to analyze and design DC biasing circuits

More information

University of Pittsburgh

University of Pittsburgh University of Pittsburgh Experiment #5 Lab Report Diode Applications and PSPICE Introduction Submission Date: 10/10/2017 Instructors: Dr. Minhee Yun John Erickson Yanhao Du Submitted By: Nick Haver & Alex

More information

Electronics EECE2412 Spring 2017 Exam #2

Electronics EECE2412 Spring 2017 Exam #2 Electronics EECE2412 Spring 2017 Exam #2 Prof. Charles A. DiMarzio Department of Electrical and Computer Engineering Northeastern University 30 March 2017 File:12198/exams/exam2 Name: : General Rules:

More information

Phy 335, Unit 4 Transistors and transistor circuits (part one)

Phy 335, Unit 4 Transistors and transistor circuits (part one) Mini-lecture topics (multiple lectures): Phy 335, Unit 4 Transistors and transistor circuits (part one) p-n junctions re-visited How does a bipolar transistor works; analogy with a valve Basic circuit

More information

Conduction Characteristics of MOS Transistors (for fixed Vds)! Topic 2. Basic MOS theory & SPICE simulation. MOS Transistor

Conduction Characteristics of MOS Transistors (for fixed Vds)! Topic 2. Basic MOS theory & SPICE simulation. MOS Transistor Conduction Characteristics of MOS Transistors (for fixed Vds)! Topic 2 Basic MOS theory & SPICE simulation Peter Cheung Department of Electrical & Electronic Engineering Imperial College London (Weste&Harris,

More information

Topic 2. Basic MOS theory & SPICE simulation

Topic 2. Basic MOS theory & SPICE simulation Topic 2 Basic MOS theory & SPICE simulation Peter Cheung Department of Electrical & Electronic Engineering Imperial College London (Weste&Harris, Ch 2 & 5.1-5.3 Rabaey, Ch 3) URL: www.ee.ic.ac.uk/pcheung/

More information

Conduction Characteristics of MOS Transistors (for fixed Vds) Topic 2. Basic MOS theory & SPICE simulation. MOS Transistor

Conduction Characteristics of MOS Transistors (for fixed Vds) Topic 2. Basic MOS theory & SPICE simulation. MOS Transistor Conduction Characteristics of MOS Transistors (for fixed Vds) Topic 2 Basic MOS theory & SPICE simulation Peter Cheung Department of Electrical & Electronic Engineering Imperial College London (Weste&Harris,

More information

ECE 310L : LAB 9. Fall 2012 (Hay)

ECE 310L : LAB 9. Fall 2012 (Hay) ECE 310L : LAB 9 PRELAB ASSIGNMENT: Read the lab assignment in its entirety. 1. For the circuit shown in Figure 3, compute a value for R1 that will result in a 1N5230B zener diode current of approximately

More information

EE 320 L LABORATORY 9: MOSFET TRANSISTOR CHARACTERIZATIONS. by Ming Zhu UNIVERSITY OF NEVADA, LAS VEGAS 1. OBJECTIVE 2. COMPONENTS & EQUIPMENT

EE 320 L LABORATORY 9: MOSFET TRANSISTOR CHARACTERIZATIONS. by Ming Zhu UNIVERSITY OF NEVADA, LAS VEGAS 1. OBJECTIVE 2. COMPONENTS & EQUIPMENT EE 320 L ELECTRONICS I LABORATORY 9: MOSFET TRANSISTOR CHARACTERIZATIONS by Ming Zhu DEPARTMENT OF ELECTRICAL AND COMPUTER ENGINEERING UNIVERSITY OF NEVADA, LAS VEGAS 1. OBJECTIVE Get familiar with MOSFETs,

More information

Concept map Introduction E lectronics and Microelectronics Engineering have been highly strengthen by the micro and nanotechnology advances which have provided a wide range of applications and solutions

More information

Xcircuit and Spice. February 26, 2007

Xcircuit and Spice. February 26, 2007 Xcircuit and Spice February 26, 2007 This week we are going to start with a new tool, namely Spice. Spice is a circuit simulator. The variant of spice we will use here is called Spice-Opus, and is a combined

More information

Revised April Unit/Standard Number. Proficiency Level Achieved: (X) Indicates Competency Achieved to Industry Proficiency Level

Revised April Unit/Standard Number. Proficiency Level Achieved: (X) Indicates Competency Achieved to Industry Proficiency Level Unit/Standard Number Electrical, Electronic and Communications Engineering Technology/Technician CIP 15.0303 Task Grid Secondary Competency Task List 100 SAFETY 101 Demonstrate an understanding of state,

More information

EXPERIMENT 12: SIMULATION STUDY OF DIFFERENT BIASING CIRCUITS USING NPN BJT

EXPERIMENT 12: SIMULATION STUDY OF DIFFERENT BIASING CIRCUITS USING NPN BJT EXPERIMENT 12: SIMULATION STUDY OF DIFFERENT BIASING CIRCUITS USING NPN BJT AIM: 1) To study different BJT DC biasing circuits 2) To design voltage divider bias circuit using NPN BJT SOFTWARE TOOL: PC

More information

Microelectronic Circuits

Microelectronic Circuits SECOND EDITION ISHBWHBI \ ' -' Microelectronic Circuits Adel S. Sedra University of Toronto Kenneth С Smith University of Toronto HOLT, RINEHART AND WINSTON HOLT, RINEHART AND WINSTON, INC. New York Chicago

More information

1.3 An Introduction to WinSPICE

1.3 An Introduction to WinSPICE Chapter 1 Introduction to CMOS Design 23 After the GDS file is generated, we can use the Gds2Tlc program to convert the GDS file back into TLC files. In the setups we must specify a directory where the

More information

OrCAD PSpice - Tutorial. TA: 黃玉龍

OrCAD PSpice - Tutorial. TA: 黃玉龍 OrCAD PSpice - Tutorial TA: 黃玉龍 r9994320@ntu.edu.tw Outline 2 Introduction Preparation Schematic Simulation Conclusion Introduction 3 OrCAD PSpice is developed by Cadence Analog circuit simulation tool

More information

DEPARTMENT OF ELECTRICAL ENGINEERING. Date: Assistant A2: PSpice 2 PC Pool

DEPARTMENT OF ELECTRICAL ENGINEERING. Date: Assistant A2: PSpice 2 PC Pool University of Applied Sciences Hamburg Group No : DEPARTMENT OF ELECTRICAL ENGINEERING Laboratory for Instrumentation and Measurement L1: in charge of the report PSpice 2 PC Pool Date: Assistant A2: Professor:

More information

Experiment # 4: BJT Characteristics and Applications

Experiment # 4: BJT Characteristics and Applications ENGR 301 Electrical Measurements Experiment # 4: BJT Characteristics and Applications Objective: To characterize a bipolar junction transistor (BJT). To investigate basic BJT amplifiers and current sources.

More information

Basic Electronics Prof. Dr. Chitralekha Mahanta Department of Electronics and Communication Engineering Indian Institute of Technology, Guwahati

Basic Electronics Prof. Dr. Chitralekha Mahanta Department of Electronics and Communication Engineering Indian Institute of Technology, Guwahati Basic Electronics Prof. Dr. Chitralekha Mahanta Department of Electronics and Communication Engineering Indian Institute of Technology, Guwahati Module: 2 Bipolar Junction Transistors Lecture-1 Transistor

More information

Common-source Amplifiers

Common-source Amplifiers Lab 1: Common-source Amplifiers Introduction The common-source amplifier is one of the basic amplifiers in CMOS analog circuits. Because of its very high input impedance, relatively high gain, low noise,

More information

ELEC3106 Electronics. Lab 4: EMI simulations with SPICE. Objective. Material. Simulations

ELEC3106 Electronics. Lab 4: EMI simulations with SPICE. Objective. Material. Simulations ELEC3106 Electronics Lab 4: EMI simulations with SPICE Objective The objective of this laboratory session is to give the students a good understanding of the possibilities a circuit simulator (as SPICE)

More information

University of Michigan EECS 311: Electronic Circuits Fall 2008 LAB 4 SINGLE STAGE AMPLIFIER

University of Michigan EECS 311: Electronic Circuits Fall 2008 LAB 4 SINGLE STAGE AMPLIFIER University of Michigan EECS 311: Electronic Circuits Fall 2008 LAB 4 SINGLE STAGE AMPLIFIER Issued 10/27/2008 Report due in Lecture 11/10/2008 Introduction In this lab you will characterize a 2N3904 NPN

More information

the reactance of the capacitor, 1/2πfC, is equal to the resistance at a frequency of 4 to 5 khz.

the reactance of the capacitor, 1/2πfC, is equal to the resistance at a frequency of 4 to 5 khz. EXPERIMENT 12 INTRODUCTION TO PSPICE AND AC VOLTAGE DIVIDERS OBJECTIVE To gain familiarity with PSPICE, and to review in greater detail the ac voltage dividers studied in Experiment 14. PROCEDURE 1) Connect

More information

BJT Characteristics & Common Emitter Transistor Amplifier

BJT Characteristics & Common Emitter Transistor Amplifier LAB #07 Objectives 1. To graph the collector characteristics of a transistor. 2. To measure AC and DC voltages in a common-emitter amplifier. Theory BJT A bipolar (junction) transistor (BJT) is a three-terminal

More information

EE 105 MICROELECTRONIC DEVICES & CIRCUITS FALL 2018 C. Nguyen. Laboratory 2: Characterization of the 741 Op Amp Preliminary Exercises

EE 105 MICROELECTRONIC DEVICES & CIRCUITS FALL 2018 C. Nguyen. Laboratory 2: Characterization of the 741 Op Amp Preliminary Exercises Laboratory 2: Characterization of the 741 Op Amp Preliminary Exercises This lab will characterize an actual 741 operational amplifier with emphasis on its non-ideal properties, such as finite gain and

More information

LTSpice Basic Tutorial

LTSpice Basic Tutorial Index: I. Opening LTSpice II. Drawing the circuit A. Making Sure You Have a GND B. Getting the Parts C. Placing the Parts D. Connecting the Circuit E. Changing the Name of the Part F. Changing the Value

More information

Revised April Unit/Standard Number. High School Graduation Years 2016, 2017 and 2018

Revised April Unit/Standard Number. High School Graduation Years 2016, 2017 and 2018 Unit/Standard Number High School Graduation Years 2016, 2017 and 2018 Electrical, Electronic and Communications Engineering Technology/Technician CIP 15.0303 Task Grid Secondary Competency Task List 100

More information

Electronic Circuits Laboratory EE462G Lab #3. Diodes, Transfer Characteristics, and Clipping Circuits

Electronic Circuits Laboratory EE462G Lab #3. Diodes, Transfer Characteristics, and Clipping Circuits Electronic Circuits Laboratory EE46G Lab #3 Diodes, Transfer Characteristics, and Clipping Circuits Instrumentation This lab requires: Function Generator and Oscilloscope (as in Lab ) Tektronix s PS 80

More information

DOWNLOAD OR READ : BASIC ELECTRONICS TRANSISTORS AND INTEGRATED CIRCUITS WORKBOOK 1 PDF EBOOK EPUB MOBI

DOWNLOAD OR READ : BASIC ELECTRONICS TRANSISTORS AND INTEGRATED CIRCUITS WORKBOOK 1 PDF EBOOK EPUB MOBI DOWNLOAD OR READ : BASIC ELECTRONICS TRANSISTORS AND INTEGRATED CIRCUITS WORKBOOK 1 PDF EBOOK EPUB MOBI Page 1 Page 2 basic electronics transistors and integrated circuits workbook 1 basic electronics

More information

Experiment No. 9 DESIGN AND CHARACTERISTICS OF COMMON BASE AND COMMON COLLECTOR AMPLIFIERS

Experiment No. 9 DESIGN AND CHARACTERISTICS OF COMMON BASE AND COMMON COLLECTOR AMPLIFIERS Experiment No. 9 DESIGN AND CHARACTERISTICS OF COMMON BASE AND COMMON COLLECTOR AMPLIFIERS 1. Objective: The objective of this experiment is to explore the basic applications of the bipolar junction transistor

More information

Dr. Charles Kim ELECTRONICS I. Lab 5 Bipolar Junction Transistor (BJT) I TRADITIONAL LAB

Dr. Charles Kim ELECTRONICS I. Lab 5 Bipolar Junction Transistor (BJT) I TRADITIONAL LAB ELECTRONICS I Lab 5 Bipolar Junction Transistor (BJT) I TRADITIONAL LAB MOBILE STUDIO LAB Before We Start A transistor is a 3-terminal device available in two configurations, NPN and PNP. The transistor

More information

ECE 454 Homework #1 Due 11/28/2018 This Wednesday In Lab

ECE 454 Homework #1 Due 11/28/2018 This Wednesday In Lab ECE 454 Homework #1 Due 11/28/2018 This Wednesday In Lab Design the Darlington push-pull amplifier specified in Lab 1: You will build this amplifier for Lab 1 so use parts that are available in the lab.

More information

Chapter 8. Chapter 9. Chapter 6. Chapter 10. Chapter 11. Chapter 7

Chapter 8. Chapter 9. Chapter 6. Chapter 10. Chapter 11. Chapter 7 5.5 Series and Parallel Combinations of 246 Complex Impedances 5.6 Steady-State AC Node-Voltage 247 Analysis 5.7 AC Power Calculations 256 5.8 Using Power Triangles 258 5.9 Power-Factor Correction 261

More information

Lab 5: Multi-Stage Amplifiers

Lab 5: Multi-Stage Amplifiers UNIVERSITY OF CALIFORNIA AT BERKELEY College of Engineering Department of Electrical Engineering and Computer Sciences EE105 Lab Experiments Lab 5: Multi-Stage Amplifiers Contents 1 Introduction 1 2 Pre-Lab

More information

How SPICE Transformed Integrated Circuit Design

How SPICE Transformed Integrated Circuit Design How SPICE Transformed Integrated Circuit Design Laurence W. Nagel Omega Enterprises Consulting Presented at ISAT/DARPA Workshop Naturally Expressed Rapid Design (NERD) Warrenton, VA August 14-15, 2014

More information